CFD Online Discussion Forums

CFD Online Discussion Forums (http://www.cfd-online.com/Forums/)
-   OpenFOAM Post-Processing (http://www.cfd-online.com/Forums/openfoam-post-processing/)
-   -   Velocity profiles near walls? (http://www.cfd-online.com/Forums/openfoam-post-processing/63900-velocity-profiles-near-walls.html)

Hectux April 23, 2009 04:01

Velocity profiles near walls?
 
2 Attachment(s)
Hi,

I ran in the last days some simulations in pipe geometries.
In ParaView I to wanted to plot the velovity profiles (y: Velovity, x: Radius).
In the center of the tube everything worked great. But near the walls I had a region where the velocity was everywhere the same.

I thought I had a problem with my simulation. So I took the tutorial cavity for icoFoam, altered it a bit to see the profile well and ran it.
The same profile. In the centre was everything good and nearer to the walls I had a jump to the wall velocity. Actually I expected a smooth raise of the velocity to the wall.

In my simulation the geometry is much smaller and the region near the wall therefore much bigger than here. Thats not what I expected or what it should be.

I attached the two pictures with the profiles and marked the regions.


Thanks for help.

Hectux April 23, 2009 09:03

Problem solved....almost.

When I use Sample from OpenFoam and import the Data to Excel I get a good smooth profile. Do not know why ParaView creates such profiles.

Any sugestions why?

santos April 23, 2009 10:09

Hi Hectux,

Try to increase the number of points in the x-y plot, and see if it helps.

Regards,
Jose Santos

Hectux April 23, 2009 14:37

Yes. Thats probably the problem. But I cannot find the funkction to increase the number of points.

With SampleDict it was no problem to set 10 oder 500 points.

mahaputra April 23, 2009 18:27

Dear Hectux

could you please teach step by step, how you work with SampleDict to plot your xy velocity profile?

im facing a similar case.

please give me help

Hectux April 24, 2009 04:46

Ok.

First there is an example file of SampleDict in $FOAM_UTILITIES/postProcessing/sampling/sample
There is a complete SampleDict file with every functions. You will find a better description in the UsersGuide of OpenFOAM.

The SampleDict is saved in the system folder. Often you have to create a file on your own:

My SampleDict is quite simple but it works well for me:
/*--------------------------------*- C++ -*----------------------------------*\
| ========= | |
| \\ / F ield | OpenFOAM: The Open Source CFD Toolbox |
| \\ / O peration | Version: 1.5 |
| \\ / A nd | Web: http://www.OpenFOAM.org |
| \\/ M anipulation | |
\*---------------------------------------------------------------------------*/
FoamFile
{
version 2.0;
format ascii;
class dictionary;
object sampleDict;
}
// * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * * //

interpolationScheme cellPoint;

setFormat raw;

sets
(
profile
{
type uniform;
axis y;
start (0 -5e-4 2e-3);
end (0 5e-4 2e-3);
nPoints 500;
}
);

surfaces
();

fields
(
U
);

// ************************************************** *********************** //

What it does: Creates a line with evenly distributed 500 points. Start point (0 -5e-4 2e-3) end points (0 5e-4 2e-3).
Thats a cut through the center of my pipe.

With fields: U

I get a file which I can import to e.g. Excel or Spreadsheet.

So I have 4 colums. First: The coordinates of my points, second: Ux component of the velocity vector in that point, third: Uy, fourth Uz.

I had to change the punctuation from "." to "," in Excel but that should be no problem, I think ;-)

santos April 24, 2009 08:35

Quote:

Originally Posted by Hectux (Post 213971)
Yes. Thats probably the problem. But I cannot find the funkction to increase the number of points.

With SampleDict it was no problem to set 10 oder 500 points.

I guess you missed it.. If you look in the Properties tab of ProbeLine filter, at the bottom you have the Resolution option with a default of 100. Try to change this value to see if it helps.

Regards,
Jose Santos

mahaputra April 24, 2009 18:33

Dear Hectux

thanks for your tutorial, thousand thanks.

regarding plotting, maybe you can use xmgrace tool

sudo apt-get install xmgrace

this software really easy to use compare excell (at least for me) :)

lth May 20, 2009 09:37

help with xmgrace
 
Hello Hectux,

I read your post and have not been able to get xmgrace to plot anything. I installed and when I run a sampledict and have sets files filled, I run xmgrace and the postprocessing window opens, however, i am not able to bring up any plots? Can you say what is needed to get the data showing?

Thanks for any advice, Lori Holmes

Hectux May 21, 2009 09:42

Sorry, I am not using xmgrace. I am still using Excel.

I suggest you write mahaputra an private message.

mahaputra May 21, 2009 09:49

Hei lth


follow this :

Use: Data/Import/ASCII. Choose the logs directory and remove '.dat' from the filter. Then you can plot whatever you like in the logs directory.


hope this help

cheers

mahaputra May 21, 2009 09:51

Quote:

Originally Posted by lth (Post 216727)
Hello Hectux,

I read your post and have not been able to get xmgrace to plot anything. I installed and when I run a sampledict and have sets files filled, I run xmgrace and the postprocessing window opens, however, i am not able to bring up any plots? Can you say what is needed to get the data showing?

Thanks for any advice, Lori Holmes

see this one:


http://www.cfd-online.com/Forums/ope...-plotting.html


All times are GMT -4. The time now is 08:11.